Stop new format from updating old drawings?

[pcnelson]

Is there a config setting, or another method, that allows me to make a modification to a drawing format and not have the new format update old drawings when they are opened? I want to add a sketch to a format, but right now it will appear on old drawings as soon as I open them. I only want the sketch on new drawings going forward. I've modified some tables on the format, and they seem to be static on old drawings and only appearwhen creating a new drawing. What did I do wrong? We are on PDMLink 10.0 M020 and Creo Elements/Pro 5.0 M130. Thanks for your help.

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[rseys]

I think that's a fault with Pro/E - Creo Parametric drawings. Better functionality would be for Pro/E-Creo drawings to be similar to old hand-drawn prints. I.e., once created, a drawing should be unalterable. Another way to say it is that a drawing should be "published". It stinks that updating a drawing format will change already-existing drawings.

To answer your question, the way we deal with this issue at my workplace is, anytime a drawing format is updated, it is given a new name.

Regards,

Randy Seys | CAD Administrator
1911 Lee Boulevard | North Mankato | MN | 56003 | mico.com
* +1 507 625 6426 | 7 +1 507 625 3212 | * nnewton@mico.com<">mailto:nnewton@mico.com>

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[TomU]

Formats are always seen "thru" the drawing, except for tables. At the time of drawing creation tables are copied from the format to the drawing. Notes, sketches, symbols, etc. on the format will always be visible thru any drawing that is using that format. This behavior argues for either NEVER making changes to a format after it's been created (new/changed formats should be copied with new names), or duplicate the format with each job so the format is job specific and no longer tied to your "library" format.

Tom U.

[MikeFoster]

This is problem is resolved if the "As Stored" configuration is used for configuration control (looking at previously released work) and the "Latest" configuration is used for new design.

Mike Foster
ATK

[pcnelson]

I might have done something wrong, but when I tried this I selected the
model, changed dependencies to As Stored and added to WS. When I opened
the drawing from the WS the format was updated.



On Wed, Aug 14, 2013 at 10:45 AM, Foster, Mike (Goleta) <-<br/>> wrote:

> This is problem is resolved if the "As Stored" configuration is used
> for configuration control (looking at previously released work) and the
> "Latest" configuration is used for new design.****
>
> ** **
>
> Mike Foster****
>
> ATK****
>
> ** **
>
> *From:* Randy Seys [

[TomU]

You said you selected the model. Assuming you mean "part" or "assembly" and not "drawing", As-Stored will bring along the dependents of the initially selected object, not the extra 'stuff' like drawings. Since the format is not a dependency of the model, it will not come out as stored, instead you will get the latest. This is not the case if you had selected the drawing itself and chosen required and 'as stored'.

This is one of the things that bugs me about Windchill. If you select something and tell it to bring along the required dependents 'as stored', any additional dependents that those initial dependents bring along don't also come 'as stored'.

Tom U.

[BenLoosli]

The other thing to watch is what is already in your workspace. If you have the latest format in your workspace, even selecting a drawing from the Product and using As Stored, in Pro/E, you will end up with the latest format not the As Saved one.

You can only have 1 version/iteration of the format in your workspace.
Pro/E will always load from memory, then the workspace before going to the Library for the format.

[pcnelson]

I think the reason is due to the config setting. It points to a network location for the formats. We tried pointing to the Windchill formats folder briefly,but for whatever reason it was very slow to open when creating new objects. So now formats are stored both locations (WC to prevent the "already exists" message). The checkout list shows the As Stored versions of the part and drawing, but includes no format. When the drawing is opened from the WS it must look to the network location rather than get the original format from WC. It looks like the cleanest method to solve this is to rename the format every time it is modified. I dont like that, but it may be what we have to do to keep the associations.

[dgallup]

One place I worked at used a huge symbol as their drawing format rather than the the format functionality. That does accomplish what you want as the symbol definition is stored in the drawing but can be updated from disk if you want the new definition. I thought it was rather weird.

One nice thing about formats updating automatically is you can change things like company logos and they will automatically get updated the next time the drawing is revised. We once went through a spell where the logo was changed 3 times in about 6 months.

In Reply to Tom Uminn:

Formats are always seen "thru" the drawing, except for tables. At the time of drawing creation tables are copied from the format to the drawing. Notes, sketches, symbols, etc. on the format will always be visible thru any drawing that is using that format. This behavior argues for either NEVER making changes to a format after it's been created (new/changed formats should be copied with new names), or duplicate the format with each job so the format is job specific and no longer tied to your "library" format.

Tom U.